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Counter-sunk holes on flat-pattern view
c_harsha
Member Posts: 15 PRO
Hello everyone,
I am writing this post to discuss on how Onshape users get around the problem of not being able to create cross-sectional forming features (like counter-sunk hole) in flat pattern of sheet metal design in Onshape. I have seen posts where it has been suggested to create conter-sunk holes after 'finish sheet metal operation', however this method doesn't go anywhere near of showing the hole in flat pattern view in drawings, which is the document shared with suppliers to manufacture the part.
I thought of a method around this. Taking counter-sunk hole as an example, I create clearnace hole(s) initially and continue to work on sheet metal design. Then, just before I do 'finish sheet metal operation', I move to flat pattern window in part studio and create a sketch with circle(s) concentric to clearance hole(s). I change between solid line - construction line, depending on position of contersunk head wrt to flat pattern view. Then I do 'finish sheet metal operation' and create countersunk at respective clerance hole positions. Later in 2-D drawing, in 'show/hide sketches panel', I select the before mentioned sketch to show visibility of the counter-sunk in flat-pattern drawing.
However, as seen in the picture above, its not really a 'hidden line font' for the outer edge of counter-sunk hole, but atleast it does the job of showing countersunk hole in flat-pattern drawing. Most of the time, our suppliers don't ask for dimensions of features on flat-pattern, and flat pattern is only used to just present how flat part will look, so they have some clear idea while manufacturing. Hence, I don't particularly look for perfect hidden lines here, however when I have more than 5 holes very near to each other, it does get a bit confusing.
Is there anyone who work on sheet-metal designs using Onshape able to get around this problem in any other (possibly better) way? This method only works for counter-sunk holes (or a bit similar features), what about other kind of features from embossing, etc.?
Does Onshape plan to roll out an update in near future enabling users to create this kind of features directly in sheet-metal design? Or in other way, providing sketch tools in 2-D drawing will solve a part of this problem.
I am writing this post to discuss on how Onshape users get around the problem of not being able to create cross-sectional forming features (like counter-sunk hole) in flat pattern of sheet metal design in Onshape. I have seen posts where it has been suggested to create conter-sunk holes after 'finish sheet metal operation', however this method doesn't go anywhere near of showing the hole in flat pattern view in drawings, which is the document shared with suppliers to manufacture the part.
I thought of a method around this. Taking counter-sunk hole as an example, I create clearnace hole(s) initially and continue to work on sheet metal design. Then, just before I do 'finish sheet metal operation', I move to flat pattern window in part studio and create a sketch with circle(s) concentric to clearance hole(s). I change between solid line - construction line, depending on position of contersunk head wrt to flat pattern view. Then I do 'finish sheet metal operation' and create countersunk at respective clerance hole positions. Later in 2-D drawing, in 'show/hide sketches panel', I select the before mentioned sketch to show visibility of the counter-sunk in flat-pattern drawing.
However, as seen in the picture above, its not really a 'hidden line font' for the outer edge of counter-sunk hole, but atleast it does the job of showing countersunk hole in flat-pattern drawing. Most of the time, our suppliers don't ask for dimensions of features on flat-pattern, and flat pattern is only used to just present how flat part will look, so they have some clear idea while manufacturing. Hence, I don't particularly look for perfect hidden lines here, however when I have more than 5 holes very near to each other, it does get a bit confusing.
Is there anyone who work on sheet-metal designs using Onshape able to get around this problem in any other (possibly better) way? This method only works for counter-sunk holes (or a bit similar features), what about other kind of features from embossing, etc.?
Does Onshape plan to roll out an update in near future enabling users to create this kind of features directly in sheet-metal design? Or in other way, providing sketch tools in 2-D drawing will solve a part of this problem.
0
Comments
Might not be that helpful "today" but the functionality was previewed at "Onshape live" so it should be coming "fairly soon".
One option would be to use this custom feature to insert a flattened version of your part and put the countersinks in here. It's obviously not ideal (and will mess up release workflows because it's a separate part) so we typically just use notes and/or show them in the formed part...
I've done this with pilot holes. Start with smaller holes at locations required.
Finish the sheet metal part then add countersink/counterbore holes at the implicit hole mate of the pilot holes.
In the drawing flat view use auto centerlines for dimensions.
Use hide edges to make the pilot holes go away.
This is assuming that laser cutter can't make countersink holes but can mark center lines for drilling.
It will make a clean DXF from flat view.
https://cad.onshape.com/documents/90f92fa3a94aec6243fe0760/w/62df10306df924ec9b11c15b/e/2e59f25704032f7c5d89cc19
Caution. The pilot holes in sheet metal model don't always come back as exactly cylindrical. Keep an eye out when selecting mates.
I'm hoping the new sheet metal function coming will do a much better job.